From Mesh Quality to CFD Accuracy

By Dr. Wolfgang Gentzsch, SimOps Foundation, In-depth analysis inspired by the SimOps 101 Blog on Mesh Generation in CFD.

Understanding Discretization Error, Convergence and Numerical Uncertainty

Computational Fluid Dynamics has become one of the most powerful tools in modern engineering. Aircraft, automobiles, turbomachinery, buildings, medical devices and countless other products are designed and optimized with the help of CFD.

Yet every CFD simulation begins with an approximation.

The continuous physical domain must be divided into a finite number of computational cells, and the governing partial differential equations must be transformed into a system of discrete algebraic equations that can be solved on a computer.

That transformation is where the mesh enters.

For many engineers, mesh generation is still regarded primarily as a preprocessing task: create the geometry, generate sufficiently small cells, check skewness and aspect ratio, and then start the solver.

But numerical analysis tells us something much more fundamental: The mesh is part of the numerical method. Its resolution, topology, smoothness, orthogonality, stretching and relationship to the underlying physics directly influence the discretization error, convergence behavior, computational cost—and ultimately the credibility of the CFD result.

This is not merely a theoretical observation. Decades of numerical-analysis research, together with more recent CFD studies, continue to demonstrate that mesh quality can change both the magnitude of numerical error and the observed convergence behavior [1].

From continuous physics to a discrete solution

The Navier–Stokes equations describe continuous physical phenomena. A CFD solver, however, does not solve those equations directly. Instead, the domain is discretized, derivatives and fluxes are approximated, and the continuous equations become a finite algebraic system. This inevitably introduces discretization error.

A useful conceptual decomposition is:

Physical model error → Is the mathematical model appropriate?

Discretization error → Does the numerical discretization adequately represent the governing equations?

Iterative error → Has the algebraic/nonlinear system actually been solved sufficiently accurately?

Numerical round-off → Are finite-precision effects significant?

These error sources should not be confused. A solver can reach a very small residual while the discretization error remains large. Conversely, a highly refined mesh does not guarantee a correct physical prediction if the turbulence model, boundary conditions or other modeling assumptions are inappropriate.

Recent work on CFD validation at high Reynolds numbers reinforces this distinction: grid/discretization error, physical-model uncertainty, measurement uncertainty and differences between computational and experimental conditions all contribute to the total uncertainty, [3]. This leads to one of the most important statements in CFD:

A converged CFD solution is not necessarily an accurate CFD solution.

Consistency, stability and convergence

Classical numerical analysis provides the theoretical foundation for understanding this problem. A discretization should be consistent: as the characteristic mesh spacing (h) becomes smaller, the discrete equations should approach the governing continuous equations. It should also be stable: numerical errors should remain controlled rather than growing without bound. Under the assumptions of the classical Lax Equivalence Theorem for well-posed linear finite-difference initial-value problems, consistency and stability are equivalent to convergence.

In other words: Consistency + Stability → Convergence

The practical CFD problem is considerably more complicated, however. Industrial CFD commonly involves nonlinear Navier–Stokes equations, turbulence models, finite-volume or finite-element discretizations, unstructured and hybrid meshes, complex geometries, moving boundaries, multiphase flows and highly anisotropic physical structures. The classical theory therefore provides the foundation—but not a simple universal "mesh quality number."

Mesh quality is not one number

Terms such as skewness, non-orthogonality, aspect ratio, stretching and expansion ratio are familiar to every CFD practitioner. But it is dangerous to interpret them as universal indicators of solution quality.

Consider aspect ratio. A cell with an aspect ratio of 100 may sound terrible. But if it lies in a well-resolved boundary layer and is strongly stretched in the physically appropriate direction, it may be exactly what the simulation requires.

On the other hand, a cell with a seemingly excellent aspect ratio can still be inadequate if the flow feature of interest is unresolved. The same principle applies to orthogonality and skewness.

The relevance of a mesh-quality metric depends on how the solver discretizes the governing equations. Ansys' CFX documentation explicitly makes this point: the relevant definitions and acceptable ranges for orthogonality, expansion and aspect ratio are closely related to the discrete approximations employed by the particular solver, [4].

This is an important lesson:

There is no universally "good mesh." There is only a mesh that is appropriate—or inappropriate—for a particular numerical method, physical problem and quantity of interest.

What happens when the mesh is poor?

Poor mesh quality can influence CFD in several ways.

Skewness and non-orthogonality

They can introduce additional errors into gradient, diffusion and flux approximations. Research on unstructured finite-volume methods has shown that mesh-induced skewness can degrade numerical fidelity, accuracy and even the formal order of convergence [5]. Recent research on multiphase flow goes further: non-orthogonality errors can create force imbalances at interfaces and generate artificial velocities, [6].

Abrupt cell-size changes

Rapid changes in cell size can increase interpolation errors and adversely affect the propagation of information through the numerical stencil.

Poor near-wall resolution

If the mesh does not resolve the relevant boundary-layer physics—or is inconsistent with the wall treatment—the error may dominate quantities such as wall shear stress, separation and heat transfer.

Local defects can have global consequences

This is particularly interesting. A small number of poor-quality cells does not necessarily mean that only a small part of the solution is affected.

A detailed study of flow around a square cylinder found that moderately skewed near-wall cells located upstream could influence the boundary layer, separation and vortex shedding farther downstream. In contrast, similar skewness near the trailing edge had a much smaller effect, [7].

So the question is not simply: How many bad cells do I have?

It is: Where are they, and what physical information passes through them?

Mesh refinement and the limit (h → 0)

The fundamental idea behind grid convergence is beautifully simple. As the characteristic mesh size (h) decreases, h → 0, the numerical solution should approach the exact solution—assuming the discretization is appropriate and the required mathematical conditions are satisfied. In practice, of course, we cannot use an infinitely fine mesh.

A useful engineering approach is therefore to perform simulations on a systematically refined family of meshes.

For a quantity of interest, ϕ,

ϕ_h​ = ϕ₀+ Ch^p+ O(h^p+1),

where:

• ϕ₀ is the extrapolated solution,

• C is a problem-dependent constant,

• p is the observed order of convergence.

This provides the basis for methods such as Richardson extrapolation and the Grid Convergence Index (GCI).

Eça and Hoekstra [2] developed a rigorous procedure for estimating numerical uncertainty from grid-refinement studies, particularly emphasizing the need to distinguish well-behaved convergence from irregular or oscillatory behavior, [3].

"Mesh independence" is not quite the right concept

Engineers often say: "The solution is mesh independent." Strictly speaking, it never is. The solution remains a numerical approximation. A better statement is:

The estimated discretization uncertainty in the quantity of interest is sufficiently small for the engineering purpose. This distinction matters enormously.

A pressure drop might have become insensitive to further refinement while a local wall shear stress, separation point or peak temperature is still strongly mesh dependent. A recent review of mesh adaptation research emphasizes exactly this point: refinement can be driven either by local physical features or by the error in a specific quantity of interest, including through goal-oriented adjoint methods, [5].

The quantity of interest changes everything

Suppose we simulate flow through a complex component. What are we trying to predict?

• Total pressure loss?

• Lift?

• Drag?

• Heat-transfer coefficient?

• Maximum temperature?

• Wall shear stress?

• Separation location?

• Acoustic pressure?

The mesh required for one quantity may be inadequate for another.

Therefore, mesh convergence should not be treated as an abstract property of the entire simulation. It should be evaluated against the engineering quantities that actually matter. This is one reason why modern mesh-adaptation research is moving toward feature-based and goal-oriented approaches, rather than simply refining the entire domain uniformly [8].

More cells are not always the answer

The obvious reaction to mesh sensitivity is: "Just make the mesh finer." But this creates another engineering problem. More cells mean:

More memory → More compute time → More energy consumption → Higher cost

And if poor mesh quality causes slow convergence, the situation can become even worse:

Poor mesh → larger discretization error → slower iterative convergence → more solver iterations → greater computational cost → potentially less reliable result.

This is where mesh quality, numerical accuracy and HPC efficiency become one problem.

The next generation: adaptive meshes

One of the most interesting developments in recent CFD research is therefore not simply generating finer meshes—but generating better meshes where they matter. Modern mesh-adaptation approaches increasingly combine:

• error estimation,

• local refinement,

• anisotropic refinement,

• feature detection,

• solution-based adaptation,

• and goal-oriented adjoint methods.

A 2025 review of CFD mesh adaptation identifies feature-based approaches and goal-oriented adjoint methods as two major families of modern adaptation strategies [8]. Recent research is also exploring hybrid-mesh interfaces and a-priori error estimators derived from truncation-error analysis to improve the placement and quality of transitions between different mesh types, [10].

And the frontier is moving further still: researchers are experimenting with machine learning approaches that attempt to reduce spatial discretization error even on relatively coarse CFD meshes, [10].

The important point, however, is that these techniques do not eliminate the need for numerical verification. They make intelligent mesh generation possible. They do not make mesh verification unnecessary.

From mesh generation to Simulation Operations

This brings us back to a topic that is increasingly important in modern engineering:

Simulation Operations or SimOps.

A mesh should not be treated as an ephemeral preprocessing artifact that disappears once the solver starts. It is part of the provenance of the engineering result. For a reproducible CFD simulation, we should be able to identify:

• geometry version,

• mesh generator and version,

• meshing parameters,

• cell count and topology,

• mesh-quality statistics,

• boundary-layer resolution,

• y+,

• solver version,

• numerical schemes,

• convergence criteria,

• quantity of interest,

• refinement strategy,

• grid-convergence results,

• and estimated numerical uncertainty.

This turns mesh generation into a traceable component of the complete simulation lifecycle. And this is increasingly important as simulation moves into automated workflows, HPC environments, AI-assisted engineering and digital twins.

The real question is not "Is my mesh good?"

Perhaps the most important lesson from decades of numerical CFD research is that there is no single answer to the question: "Is this a good mesh?"

A better sequence of questions is:

Is the mesh appropriate for the physics?

Is the discretization scheme appropriate for the mesh?

Are the important physical gradients adequately resolved?

Has the iterative solution converged sufficiently?

Does the solution exhibit grid convergence?

What is the estimated discretization uncertainty in the quantity of interest?

And finally:

Can the mesh, numerical method and resulting uncertainty be reproduced and traced back to the engineering decision?

That is where mesh generation stops being merely preprocessing. It becomes part of engineering simulation operations.

Conclusion

A CFD result is never simply the output of a solver. It is the result of a chain:

Geometry → Mesh → Discretization → Numerical Solution → Convergence → Verification → Validation → Engineering Decision

A weakness at any point in this chain can compromise the final result. Mesh quality therefore matters—but not because every mesh must satisfy a universal collection of geometric thresholds. It matters because the mesh determines how the continuous physics is represented by the numerical method. The most reliable CFD practice is consequently not:

"Generate the finest mesh possible."

It is: "Generate a mesh appropriate to the physics, the numerical method and the quantity of interest—and demonstrate that the resulting numerical uncertainty is acceptable."

That is the real meaning of mesh quality. And perhaps the most important evolution taking place today is that we are moving from mesh generation toward mesh intelligence: meshes that are physics-aware, error-aware, goal-oriented, adaptive, reproducible—and increasingly integrated into the complete Simulation Operations lifecycle.

References

1. Katz, A. & Sankaran, V., Mesh quality effects on the accuracy of CFD solutions on unstructured meshes, Journal of Computational Physics, 2011.

2. Eça, L. & Hoekstra, M., A procedure for the estimation of the numerical uncertainty of CFD calculations based on grid refinement studies, Journal of Computational Physics, 2014.

3. Knopp, T. et al., Errors and uncertainties in CFD validation for non-equilibrium turbulent boundary layer flows at high Reynolds numbers, Journal of Turbulence, 2024.

4. Ansys Help, https://ansyshelp.ansys.com/public/Views/Secured/corp/v242/en/cfx_mod/i1323480.html

5. Hill, S., at al. Boundedness-preserving implicit correction of mesh-induced errors for VOF based heat and mass transfer, Journal of Computational Physics, 2018.

6. Liu Jun, et al., A residual-based non-orthogonality correction for force-balanced unstructured volume-of-fluid methods, The European Physical Journal Special Topics, 2026.

7. Luca, B., et al, Effects of cell quality in grid boundary layer on the simulated flow around a square cylinder, Computers & Fluids, 2022.

8. Guglielmo Vitarelli, et al., Review of Mesh Adaptation Technology Applied to Computational Fluid Dynamics, Fluids, 2025.

9. Lazaris, P., et al., Generation and a priori evaluation of different hybrid mesh interfaces for flow simulations, Computers & Fluids, 2026.

10. Gonzalez-Sieiro, J., et al., Reducing spatial discretization error on coarse CFD simulations using an openFOAM-embedded deep learning framework, Engineering with Computers, 2024/2025.